CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Help on VOF boundary conditions

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2007, 10:36
Default Help on VOF boundary conditions
  #1
Kelly
Guest
 
Posts: n/a
Hello,

I try to use VOF to model flow through a channel/detention pond with weir as outlet. It's 2 phases:Inlet I air and Inlet II water (air in the top and an initial water depth in the channel before the weir).I am pretty sure about velocity inlet and wall boundary conditions. I wonder what boundary conditions can I apply in the top air portion (pressure outlet?)and weir outlet? I am using Fluent version 6.0.

Thanks for your attention.

Kelly
  Reply With Quote

Old   August 4, 2007, 08:02
Default Re: Help on VOF boundary conditions
  #2
msureshkumar
Guest
 
Posts: n/a
Try with open channel option
  Reply With Quote

Old   August 4, 2007, 19:20
Default Re: Help on VOF boundary conditions
  #3
Kelly
Guest
 
Posts: n/a
Dear msureshkumar:

Thank you for your reply. But FLUENT 6.0 doesn't have open chanel option? Do you know any other way?

Kelly

  Reply With Quote

Old   August 7, 2007, 07:22
Default Re: Help on VOF boundary conditions
  #4
rafal
Guest
 
Posts: n/a
Hi kelly, For such a model you can use for both surfaces presure outlets. If the weir outlet is only partialy filled with water you can also try setting the top cover as a wall and weir outlet as a presure outlet. It should help with reversive flow at the cover that will probably apear if you will simutale it with the first option. rafal
  Reply With Quote

Old   August 7, 2007, 10:45
Default Re: Help on VOF boundary conditions
  #5
Kelly
Guest
 
Posts: n/a
Thank you for your help, rafal. I tried as you said,however there are "reverse flow and turbulent viscosity limited to viscosity ratio***" warnings even if I extended the domain downstream. Do you have any suggestions to remove this? By the way it is a 2D problem and a broad-crested weir with the same width as channel.

I have one more question to ask about. In setting the initial values,how to determine Gauge pressure and water volume fraction? Are they mean values of the whole domain?

Kelly
  Reply With Quote

Old   August 7, 2007, 11:41
Default Re: Help on VOF boundary conditions
  #6
rafal
Guest
 
Posts: n/a
Hi Kelly.

I am not sure if your problem is a steady or unsteady. As I imagine the problem with computations is caused by the solver connected to not good definition of a problem and i think it will help to try first to define better initial conditions. It would be good to fill the domain with the water to the level of weir top . to do this you have to:

1: adapt a region of a quad shape region/adapt... 2: fill this region with water solve/initialize/patch...

make sure also that operating presure location is where air phase is. At the outflow use the pressure of the operating conditions and before adapting region initialize with setting 'compute from...' and chose outflow.

good luck, rafal.

  Reply With Quote

Old   August 11, 2007, 12:29
Default Re: Help on VOF boundary conditions
  #7
Kelly
Guest
 
Posts: n/a
Hi,rafal:

The problem is unsteady.I tried as you suggested:Adapt a region then patch with vof=1; Set the open air as pressure outlet BC. The result seems not right. Most of water run to the Open air domain boundary not to the outlet. Do you know what's the possible reason? Thanks a lot for your help!

Kelly

  Reply With Quote

Old   August 13, 2007, 05:37
Default Re: Help on VOF boundary conditions
  #8
rafal
Guest
 
Posts: n/a
Kelly, It is hard to say without seeing results but there os one possible reason. If the open air domain is above the water (and outlet) check your gravity settings. if the y axis is direcetd up, you should set negative gravity acceleration (wich is not default).

Rafal
  Reply With Quote

Old   August 13, 2007, 10:16
Default Re: Help on VOF boundary conditions
  #9
Kelly
Guest
 
Posts: n/a
Thanks for your great help, Rafal. You are right. I can't believe I made such an obvious mistake!

Kelly
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
boundary conditions in FLUENT VOF for open channel flow newcomer Fluent Multiphase 19 August 25, 2013 09:05
Impinging Jet Boundary Conditions Anindya Main CFD Forum 24 January 11, 2012 13:40
CFX doesn't continue calculation... mactech001 CFX 6 November 15, 2009 21:25
Concentric tube heat exchanger (Air-Water) Young CFX 5 October 6, 2008 23:17
VOF and setting boundary conditions dave00001 FLUENT 0 January 25, 2008 12:37


All times are GMT -4. The time now is 15:43.